Hello,

Anyone knows a newbie/hobbist friendly library for Eagle?

In my particular case, I would like to have some parts with bigger pads.
I've attached a screenshot from Eagle. I thought that transistor pads weren't that small until I printed the layout. That transistor has extremely small pads for my soldering experience. I also would like to have those pads "in line" and not in a "triangular" form but I didn't find any library (only default ones) with a package like that.

I also found editing libraries are not so straight forward...


Suggestions are very welcomed!

Thank you

 

The library search function of Eagle is one of its weak points, but it works fine, once you get used to it. You can search just packages. For example, from the Eagle control panel, click on Library, click on transistor, then scroll down to see just the packages, then click on the various TO-92 packages. You will see some are in-line and others are not.

You have two choices: 1) You can fiddle around, find components with the pad arrangement that you want, use them and simply re-name them in your schematic; or 2) Learn to modify a component and create an alternative package.

I prefer the second method. First create your own library (I use 1<name> so it is first in the list). Then copy the component you want to modify into that library, modify it, and save the alternative version in the same library. The advantage to doing that is that when you update, all of the Eagle libraries are updated. Then you only need to move your private library to the updated version instead of having to go back and modify a large number of components in the updated Eagle libraries.

If you are having problems modifying a component, please say where you are getting stuck and we can help.

John

Edit: Was just playing with a new schematic in Eagle. If you need an NPN transistor, in the add component dialog, click on transistor, then *NPN, then scroll down the packages (right-side panel) and you will find both linear arrangements. Click on the one you want and add it to our schematic. When you need another of the same type, just use the copy button.

 

1) Click the DRC icon on the toolbar (near the bottom), or click on Tools -> Drc...
2) On the popup dialog, click the Restring tab.
3) Under "Pads", change the % to anywhere between 25 and 100. Use the same for top/bottom.
4) Click "Apply", and see your pads change size according to what you've selected.

 

It's really not so bad adding new parts to the library once you get the hang of it. It does take some fiddling around to learn it though.

Sparkfun has a pretty good Eagle tutorial on their website:
http://www.sparkfun.com/commerce/tutorial_info.php?tutorials_id=108

It certainly doesn't cover every option, but you probably don't need many of them.

One thing that can "bite" you really hard is if you fail to use the Erc function regularly. Use it early, use it often, and fix all of the errors before you start in on making a board. If errors exist, the "air wires" won't be showing connections properly, and you won't know all of what needs to be routed.

Once you have created a board from a schematic, make certain that you always have both the schematic and the board open when making changes to either one. If they get out of sync with each other (Erc will tell you if they are in sync or not), your life will be very unpleasant. The usual solution is to delete items until they ARE in sync, and then proceed from there - if you haven't used Erc regularly, it may be easier to just delete the board file and start over.

There is a ULP named Autoplace_v3.ulp available on the Cadsoft website. This is handy when you're first creating a board from a schematic. Open the autoplace ulp in the schematic editor, and it will arrange the parts in the board to be in the same location as the schematic.

Use symbols from the supply libraries to provide power/ground to your ICs. Many will automatically connect the pins if you place the correct supply symbol(s) on your schematic; for example VDD, VSS, GND, +V, -V, etc. Don't forget that you will also need to place wirepads or add connectors and connect them to supply symbols - or your finished board won't have any place to connect power and ground.

 

Thank you so much for all these useful tips!

Pads are now larger. My next step will be to learn how to make my own library.
But If you don't mind, I have another question:

Im using a J201 (N channel JFET). I found the package I want to use but I dont know why I can't use it.
This is the package: http://i195.photobucket.com/albums/z259/Pongidae/TO92.jpg
Its available for NPN/PNP transistors but not for JFET. Any JFET in "transistors-fet" library has a component (schematic) with that package (board). I tried to change J201's package but TO92- doesn't appear in the list. I also tried by browsing libraries to add package to board but I get the following error: "Can't backannotation this operation! Please do this in the schematic"

Any suggestion?

Thanks again for your help!


Edit:
I also find these two libraries. Maybe could be useful for someone who's reading this post:
http://www.opencircuits.com/SFE_Footprint_Library_Eagle
http://github.com/jkantarek/Eagle-Libraries

 

Three alternatives:
1) Draw the schematic using the NPN or PNP device and "just remember " it is wrong.
2) After you are sure everything on the board is right, copy and save the schematic to a different file, then delete the schematic. That will break the board-schematic link so you can do whatever you want on the board. The sync between board and schematic will be permanently broken.
3) Make a new device or a new variant of the JFET.

#3 is the best option. #1 is a doable, quick fix until you get more familiar with Eagle. #2 will allow you to change the package, but you WILL regret doing it. Getting a board and schematic back into sync after breaking the link is almost impossible to do.

John

 

I got really confused on a similar issue just a few weeks ago. I did a Keystone Cops type drill in my transistor library. It was not pleasant.

Note that when a TO-92 package transistor is drawn face-down like the one you showed, the pads are numbered left-to-right, starting from 1. So, the leftmost pin will be #1 when the flat face is towards the bottom of your screen.

You CAN change the package of an existing component.

1) Add the new package to the library that the component exists in.
2) Connect the device to the package using a different name. Make absolutely certain that you have the pin connections correct.
3) Add a device to the schematic, using the same component. Eagle will query you that there is an existing component of the same name, update it?
4) Click yes. Eagle will tell you to run a DRC. Close the dialog and hit ESC to avoid adding the updated component.

You should now be able to use the CHANGE-> PACKAGE command to select your new package on the existing component.

 

Sparkfun library is great! Download the library and their shortcuts. Sparkfun caters heavily to the hobbyist/tinkerer so their library pretty much has everything you will need. When I design stuff I get 80% of my parts from that library